# How to design a PCB to connect the GSM modem with 50Ohm track impedance?

In the system integration manual of the Leon G100 GSM modem (http://www.u-blox.com/images/downloads/Product_Docs/LEON-G1-G2_SystemIntegrationManual_(UBX-13002023).pdf) it’s written to carefully design the 50 Ohm micro strip or stripline on the pcb (“The transmission line up to antenna connector or pad may be a micro strip or a stripline. In any case must be designed to achieve 50 Ω characteristic impedance”). I design a 2-layer pcb and before I got to chapter 2.2.1.1 of the mentioned document I carelessly attached the ANT with the signal pin of the SMA.

I cannot use the stripline as it’s a 2-layer PCB, instead I used a coplanar waveguide with ground. Using a KiCad Pcb Calculator I ended up with the following conclusions: to have 50 Ohm at FR4 PCB of 1.5mm thickness and freq of 900MHz it has to be a 1.25mm wide path separated from the gnd paths by 0.25mm. The Electrical length 22 degrees.

And here I have some questions: - for which frequency, 900 or 1800MHz shall I calculate the parameters? - what is the 22 degrees electrical length about?. This value increases proportionally with frequency and at 1800MHz I get 44 degrees - how shall I design the vias for the gnd and sma signal pin? As far as I know the SMA connector is “through pcb” not SMD.

The electrical length is the phase shift that the design frequency experiences when travelling down the trace. In this case, it is irrelevant. For some designs, these delays must be known adjusted to specific values. Quarter wave transmission lines of specific impedances can be used for impedance matching and in the construction of various RF components. For this, you need an electrical length of 90 degrees. In your case, the length is irrelevant. For the ground vias - just position them in some what that they don't interfere with the impedance controlled trace. The signal via probably won't be very close, but at 1800 MHz, it's too small relative to the wavelength to be much of a problem. I wouldn't worry about the connector too much either for the same reason. At 2 GHz, the wavelength is about 15 cm. If any 'discontinuities' are less than 1 cm (1/16 wavelength), you should be fine.

For which frequency, 900 or 1800MHz shall I calculate the parameters?

You should try to make a design that meets the requirements at all of the frequencies you are using.

This will probably not be too difficult because the characteristic impedance won't change much with frequency.

what is the 22 degrees electrical length about?

The electrical length is the phase difference between the input and output of the transmission line.

It's given by $\frac{lf}{v}$, where l is the physical length of the line, f is the operating frequency, and v is the propagation velocity. This also shows why it increases with frequency.

If your source and load are well-matched, this does not affect the behavior of your system very much.

how shall I design the vias for the gnd and sma signal pin?

Make sure the ground pins of the connector have short, low-impedance, connections to the return path of your transmission line. If you connect your ground planes (on each side of the trace for CPW) to the vias that the connector's ground pins go through, you will be fine. At your frequencies, you should be fine using thermal relief on these pads to make soldering easier.

If you put a through hole connector on the opposite side of the board from the trace, though, it miimizes the transmission line stub from the "extra" part of the connector center pin, so this is preferred if you can do it.

Surface mount connectors are also available, and they are designed to be on the same side of the board as the trace, but they are not as physically robust as through-hole connectors.